Hello all,
I need a bit of help with the modelling of a capacitors impedance. Namely, the Murata GRM035R60J475ME15#. I am trying to get from the simulation a similar curve with the |Z| curve depicted at:
https://ds.murata.co.jp/simsurfing/mlcc.html?reqtype=open_parts&partnumbers=%5B%22GRM035R60J475ME15#%22%5D&oripartnumbers=%5B%22GRM035R60J475ME15#%22%5D&graphop=mainall&focuspartnumberonlist=true&lcid=en-us

However, I cannot get the right "parasitic" elements of the capacitor model that would result in the same curve. I have loaded in the GRM035R60J475ME15#_model.zip file which contains:
- the .asc simulation file (including the capacitor parameters I am currently using)
- the .plt file so as to configure the plot with the limits similar to the plot shown on the Murata website (for easier visual comparison of the plots)
- an .emf picture file indicating which areas of the curve I am having trouble with

I would greatly appreciate some help with this model. Whereas I am able to easy manipulate the point of the minimum impedance at 5GHz (by changing the ESR and the series inductance), the other elements are more difficult to adjust to my liking.
For example:
- I can hardly make the impedance at low frequency (100Hz) bulge without changing the capacitance itself, which, however, needs to be fixed at 4.7uF.
- I cannot make the curve in the simulation simultaneously go through the following two points (through which the curve indicated  on the Murata website does go through):  0.8Ohm @ 1GHz and 4.7Ohm @ 6GHz


Best Regards,
Cristian

In your .asc, you use a voltage source instead of a current source. Is this what you intend?

Le 01/07/2024 à 17:10, Berceanu Cristian via groups.io a écrit :

Hello all,
I need a bit of help with the modelling of a capacitors impedance. Namely, the Murata GRM035R60J475ME15#. I am trying to get from the simulation a similar curve with the |Z| curve depicted at:
https://ds.murata.co.jp/simsurfing/mlcc.html?reqtype=open_parts&partnumbers=%5B%22GRM035R60J475ME15#%22%5D&oripartnumbers=%5B%22GRM035R60J475ME15#%22%5D&graphop=mainall&focuspartnumberonlist=true&lcid=en-us

However, I cannot get the right "parasitic" elements of the capacitor model that would result in the same curve. I have loaded in the GRM035R60J475ME15#_model.zip file which contains:
- the .asc simulation file (including the capacitor parameters I am currently using)
- the .plt file so as to configure the plot with the limits similar to the plot shown on the Murata website (for easier visual comparison of the plots)
- an .emf picture file indicating which areas of the curve I am having trouble with

I would greatly appreciate some help with this model. Whereas I am able to easy manipulate the point of the minimum impedance at 5GHz (by changing the ESR and the series inductance), the other elements are more difficult to adjust to my liking.
For example:
- I can hardly make the impedance at low frequency (100Hz) bulge without changing the capacitance itself, which, however, needs to be fixed at 4.7uF.
- I cannot make the curve in the simulation simultaneously go through the following two points (through which the curve indicated  on the Murata website does go through):  0.8Ohm @ 1GHz and 4.7Ohm @ 6GHz


Best Regards,
Cristian

RLshunt is on the schematic on the Help page for Capacitors.  It is a shunt resistor across Lser.

That makes it similar to the Rpar for an inductor.  When used there, it keeps the inductor's impedance from increasing indefinitely, which might help keep simulations from aborting with something like a "time step too small" error.

Cristian,

With all that said, ...

There is something else you need to be aware of, affecting you now.  SPICE inductors are perfectly ideal, as if made with superconductors that have zero resistance Rser.  But in LTspice only(?), inductors that are not coupled have a default Rser of 1 mOhm.  (That's milliohm.)  It makes them slightly more real since you can never wind an inductor with zero wire resistance unless you have superconductors handy.  Many SPICE users get fooled by simulating with ideal inductors, only to find that the real circuit can never match.  Also Rser helps slightly with simulation convergence.

Murata's "Precise" model has seven inductors in series, which adds up to 7 mOhm, though some are shunted with small resistance making it a little less.  That extra resistance gets added to the resistance of the rest of their model.  This is what increases the minimum resistance at resonance, which you noticed.  I don't think Murata had LTspice in mind when they made their model.

To fix that, you have to add "Rser=0" to each inductor.  Murata's Precise model has seven inductors (L2, L9, L10, L11, L12, L13, L14).  For example, change this line:
    L2 11 12 1.21e-10
to this:
    L2 11 12 1.21e-10 Rser=0
and do the same to the other six, and save it.

Is there a simpler way?  Yes and no.  In LTspice's Settings (Control Panel), go to the Hacks! tab and check the checkbox for "Always default inductors to Rser=0".  However, that setting affects only simulations run during the same session of LTspice, and it reverts back to Rser=1m when you close LTspice and run it again later.

Note that the default Rser=1m applies only to actual inductors, with either the inductor schematic symbol, or an inductor Netlist line.  It does not apply to embedded inductors such as the Lser of a capacitor or a voltage-controlled switch.

Andy